Milling
Contents
Introduction
With the 3-axis milling machines it is possible to manufacture 2,5D patterns and 3D surfaces. The three axis are X, Y and Z, this means the milling tool is fitted perpendicular to the XY-plane and can move in the X and Y directions as well as up and down (Z direction). The maximum travel in the X, Y and Z direction are 1200mm, 800mm and 150mm. The Isel Flatcom 3-axis milling machine is fitted with a tool changing station making it possible to use up to 5 tools within one milling job.
The 3-axis milling machines are controlled by files in a specific format. The Isel machines are controlled by Isel_NCP files. Several programs are able to create NCP-files. We use Rhino (Rhinoceros) with a MadCam plugin. The MadCam plugin calculates and creates the toolpaths and processes this information into a NCP-file. To control MadCam within Rhinoceros we use the following toolbar.
In this manual we will explain how to use the MadCam plugin. We will use different 3D files to explain different possibilites within MadCam.
First time use
When you log on for the first time on the designated computers, MadCAM seems not to be installed within Rhino. You have to follow these steps to load the MadCAM toolbar and use the correct cutters.
- In the menu go to 'Tools > Toolbar Layout ...'
- A small window pops up.
- If MadCAM is in the list, check the checkbox behind 'madCAM 4.1'.
- If MadCAM is not in the list, then load the menu via 'File > Open...'. Go to C:\Program Files\MadCAM 4.1\System and load MadCAM4.tb.
- If MadCAM is in the list, check the checkbox behind 'madCAM 4.1'.
- Close the window.
- The cutter files are write-protected. Copy the folder C:\Program Files\MadCAM 4.1\Cutters\MadCAM-Cutters to your Desktop or to My Documents.
- Go to 'Tools > Options...' In the left pane go to MadCAM settings and choose 'Isel_NCP_BK.txt' as Post-processor and choose your copied cutter folder as your Default Cutter Folder.
- Close the window with OK.
More steps are needed to be sure that settings truly are correct.
- Make a simple Solid Box.
- Click on
and select the box and finish with Enter.
- Click on
and choose the 'Post Processor and Tool Library' tab.
- Choose the same settings as above for the 'Default Post Processor' and 'Default Tool Library' if the settings are different.
- Now you can remove the box just created ans start with the real work.
Preparation
To explain the procedures we use an example file of a lightbulb as shown at the right of this page. At first we want to position the solids and/or surfaces in a way that we can easily control the point where we want the milling machine to start. In this example we use the origin (0,0,0) as our startpoint. The easiest startpoint to position the cutter in the Isel Flatcom milling machine is one of the upper corners of the material to be milled (mostly high density polyurethane foam). In Rhinoceros this means we want to position one of the upper corners of our 'virtual block of foam' at the origin (0,0,0).
The first step we have to do is select the solids and/or surfaces to prepare them for toolpath calculation. Do this by clicking on the folowing button and selecting the solids and/or surfaces.
A box will appear around the solids and/or surfaces as shown in the second image shown at the right of this page. Furthermore a new layer will be created called 'Box/Workpiece'
Select cutting tool
For different procedures we can use different cutters. A curved surface will have the best finish with a cutter with a ball end. A flat surface will have a better finish with a flat end cutter. The best finished result for surfaces will be achieved with bigger cutter radii, however a bigger cutter radius might sometimes be impossible because of narrow spaces that need to be detailed as well.
To select a cutter use the following button on the main MadCam toolbar.
The following interface pops up.
In this cutters window you are able to choose from the available cutters. In this example library we show a ball end 6mm cutter and a flat end 6mm cutter wich we can select for our toolpath creation. Although there are quite a few parameters the only parameter that you might want to change is the 'Tool number' in case you are going to use more than one cutter tool. You can however only select one cutter at a time, you will have to create a toolpath for this cutter prior to selecting the second cutter (Tool number 2).
Create box/workpiece
Altough we have already selected the solids and/or surfaces we need to decide on a few more options. By clicking the following button on the main MadCam toolbar we enter the regions toolbar, where we can select the actual areas to be milled.
In the regions toolbar we have four options.
By clicking the first button we can create our box/workpiece. For most milling jobs creating a box/workpiece will be sufficient.
The following dialog-box pops up.
At first we only have to decide if we want the box to just enclose the solids and/or surfaces or if we want the box to also enclose close the cutter radius. In this case we chose to also enclose the cutter radius for a smooth finish near the box edge. By pressing OK we adjust the box to a slightly bigger box in the XY-plane, wich also encloses the cutter radius (as shown in the image on the right).
Repositioning
The problem however is the position of the box in relation to the origin. So we will have to move the box and the solids and/or surfaces in a way that your desired startpoint will be the origin (0,0,0). After moving the box and the solids and/or surfaces we need to rebuilt the box. This means that we will have to completely delete the layer 'Box/Workpiece'.
Now reselect the solids and/or surfaces and recreate the box the same way we did before. The result in Rhinoceros now looks like the screencapture shown on the right. The file is now ready for the next step: selecting the cutting tools.
Defining regions
In most cases defining the box/workpiece would be sufficient, but in some cases only parts of the box/workpiece need to be milled. To do this we need to enter the regions menu again.
Besides the box/workpiece button we have three other buttons.
By clicking the second button we enter the clipping planes menu.
The following dialog box pops up.
In the clipping planes menu we can limit our milling area vertically. If for example we want to mill just the upper half of the model, we set the Z Top plane above the solids and/or surfaces and the Z Bottom plane at 50% of the total hight of the solids and/or surfaces. Now the machine will only mill the solids and/or surfaces between the two planes.
In the XY-plane we can also define areas to be milled. We do this by drawing curves around the areas to be milled (the Z position of the curves has no influence on the outcome). After creating the curves we click the following button.
We select the the curves that define the the boundaries of the model and right-click or press enter. This option can best be used when all the milling will be within the boundary. If any milling should be done outside the boundary it's best to use the curve milling options.
By clicking the following button we deselect the curves.
3D milling
For the explanation of the 3D milling we will again use the lightbulb file. After repositioning everything to the desired coördinates, selecting the solids and/or surfaces, creating a box and selecting a cutter tool, we can start creating a toolpath. By clicking the following button on the main MadCam toolbar we enter the 3D Toolpath toolbar.
In the 3D Toolpath toolbar we have four options: roughing, z-level finishing, planar finishing and pencil tracing.
Roughing
Roughing is a fast way of milling the basic (rough) shape. It takes away excess material before finishing. For roughing we press the following button in the 3D Toolpath toolbar.
The following interface pops up. In the roughing window we can adjust several parameters. Roughing works through via preset steps to remove excess material.
In the 'Step Size' tab we can adjust the step down. The maximum 'StepDown' at one time is the same as the cutting length of the cutter allready set in the cutters window. The maximum 'StepOver' is the cutter diameter. Increasing the 'StepDown' and/or the 'StepOver' decreases the milling time, but leaves a rougher finish. The 'Stock To Leave' works as a surface offset. Setting this here will also effect the z-level finishing and the planar finishing. THIS IS NOT A SAFETY MARGIN FOR ROUGHING!
The 'Direction' tab holds options for movement strategies. Here you can choose the strategy in which you want the cutter to remove the excess material. In most cases 'ZigZag' is the fastest.
The parameters in the 'Traverse' tab are allright for most cases.
After adjusting the parameters we click on OK. MadCam now begins calculating the toolpath. When the toolpath is calculated MadCam creates in this case a new layer called 'ROUGHING-flat end 6mm_0-Group01' and draws the toolpath in Rhinoceros so we can visually check the toolpath (see example image on the right).
Z-level finishing
Z-level finishing is ideal for near perpendicular surfaces. By making small steps down the near perpendicular surfaces will have a smooth finish. Click the following button for entering the z-level finishing menu.
The following window pops up.
The stragety of z-level finishing is simular to the strategy of roughing. Therefore the most important parameter is the 'StepDown'. Smaller 'StepDown' results in a smoother finish. The 'Angle Limit' defines surfaces to be milled with z-level finishing. A value of 90 degrees means that all surfaces will be milled with z-level finishing. A smaller value (e.g. 70 degrees) means that surfaces with a small angle to the XY-plane (up to 20 degrees) will not be milled with z-level finishing. To make sure that all surfaces are milled when using z-level finishing together with planar finishing make sure that the sum of the angle values is more than 90 degrees. The default settings usually result in a smooth finish.
Settings at other tabs in the z-leveling window have little effect on the finished product. In most cases these settings can be left in their default settings.
After clicking OK, MadCam will calculate the toolpath for z-level finishing. A new layer called 'Z_LEVELS-ball end 6mm_1-Group02' will be added and the z-level finishing toolpath will be drawn in Rhinoceros (see image at the right).
Planar milling
Planar milling is ideal for near horizontal surfaces. By zigzagging and gradually moving sideways over the surface a smooth finish can be achieved. Click the following button for entering the planar finishing menu.
The following window pops up.
The strategy for planar finishing, zigzagging and gradualy moving sideways by smal steps, means that the 'StepOver' determines the smoothness of the finished product. A smaller 'StepOver' results in a smoother finish. The 'Angle Limit' defines the surfaces to be milled in planar finishing. A value of 0 degrees means that all surfaces will be milled in planar finishing. A bigger value (e.g. 20 degrees) means that surfaces with a big angle to the XY-plane (over 70 degrees) will not be milled in planar finishing. To make sure that all surfaces are being milled when using z-level finishing together with planar finishing make sure that the sum of the angle values is more than 90 degrees. The default settings usually result in a smooth finish.
The 'Direction' tab defines the direction of the tool movement. In 'ZigZag X' the tool moves first over the full length in the X direction before stepping over in the Y direction. 'ZigZag Y' consequently means the opposite.
Settings in other tabs in the planar window have little effect on the finished product. In most cases these settings can be left in their default setting.
After clicking OK, MadCam calculates the toolpath for planar finishing. A new layer called 'PLANAR-ball end 6mm_2-Group03' is added and the planar finishing toolpath is drawn in Rhinoceros (see the image at the right).
Pencil milling
To clean-up the overlap between Z-level finishing and planar finishing we use pencil tracing. Click the following button.
In most cases the settings can be left in their default settings.
2,5D milling
Milling 2,5D means that we are milling with a constant Z-value. Options are profiling, pocketing, facing and drilling. To explain the different procedures we use the example file shown at the right of the page. To enter the 2,5D toolbar click the following button.
The following toolbar shows.
This toolbar shows six options. The first two are advanced options for the other four options. The first button changes the curve direction. The second button allows us to move the startpoint of the curve and therefore the startpoint of the milling toolpath.
Profiling
With the profiling option we can mill contours in a model. We start by clicking the following button.
Select the profiling curves and press enter or right-click. The following window pops up.
If you have your contours drawn in the depth you want, you do not need to change any options in this tab. However, if you have your contours drawn on top of your model you have to change some values.
- Material Bottom: Fill in a negative value for the desired depth if measured from your curve. Or an absolute negative value from the top of your workpiece box. (See Options what the basis is of your depth)
- StepDown is the cutting depth for each cut, till it reaches the desired cutting depth. A higher value decreases milling time but the maximum depth depends on the cutting length of the choosen cutter and/or the density of the material to be milled.
In the 'Direction' tab you may want to change on which side of the curve the cut should be made.
In the 'Traverse' tab you might want to change the 'Radius Lead in/out' to a lower value or zero to prevent not wanted early cuts near the actual cut.
However, if we examine the toolpaths in the Profiling toolpath image at the right, we see that the toolpath of the inner curve of the letter O is actually on the wrong side of the curve. To change this we need to reverse the direction of the curve.
- Click on
from the '2,D Toolpath' toolbar
- Select the curves you want to change the direction
- Press F to change the direction and press 'Enter' when you are done.
The second image on the right shows the new toolpaths with the correct positioning.
With our example file the result will look like the following image.
Pocketing
With the pocketing option we can mill with a constant Z inside a boundary. Therefore it's the opposite of profiling. To enter the pocketing menu we click the following button.
Select the closed curves that make the pocketing curves and press enter or right-click. The following window pops up.
The settings in the 'Step Size' tab work the same as in profiling.
In the 'Step Over / Direction' tab you only might increase the StepOver to decrease milling time for this operation.
Generally, you do not need to change the settings in the 'Traverse' tab.
Examining the toolpaths in the image at the right tells us that the machine will mill the inside of the letters. This will result in the endproduct shown in the following image.
If we want the opposite to be milled, we need to add an extra curve at the edge of the Box/workpiece. After recreating the toolpath the toolpath will look like the second image at the right. And our endproduct will loook like this.
Facing
With the facing option we can mill Z-constant faces. Facing creates several profile curves starting from an outside boundary curve and moves towards inside contour curves. This operation is similar to the pocketing option. However, if we need the outer edge to be perfectly smooth the pocketing option is better. To enter the facing menu click the following button.
Select the closed curves that make the facing boundaries and press enter or right-click. The following window pops up with similar settings as in pocketing.
Looking at the image at the right we can see the difference in the toolpaths between pocketing and facing. The boundary curve is not milled as a contour in the facing option. Therefore the boundary is less smooth than the pocketing option. The endresult is more or less the same.
Drilling
With the drilling option we can drill at specified positions and with a predefined depth. To enter the drilling menu we click the following button.
We select the drilling curves (circles) and right-click or press enter. The following window pops up.
If no drill tool is loaded, the diameter and length will show "None". To load or change the drill we click the following button.
The following window pops up.
In the drill tool window we can select a drill. After selecting the tool we click ok and return to the Drill window.
The value we need to set is the drill depth. We can either specify this as an absolute Z depth or a depth relative to the surface. We click OK to start calculation of the toolpath. In our case we used an example file with a curved surface (see the image at the right). The endresult is shown in the following image. The diameter of the circles is not relevant to the diameter of the drill. MadCam will use just the center of the circle for positioning. For our understanding of the endproduct it's wise to use the actual drill diameter in our model.
Curve milling
Drawing curves as milling toolpaths or as boundaries in our model can help to create the product we want. By clicking the following button we enter the curve milling menu.
In the curve milling toolbar we have 5 options.
When using curve milling it can sometimes be nescessary to change the direction of the curve. To do this we use the following button.
Milling along curves
With the 'along curves' option we can draw curves in our model that will operate as a toolpath. To use these curves we click the following button.
The following window pops up.
In most cases the default settings are ok. Only when our cutting tool can cut less then the desired depth in one time we need to use the multiple Z-cut option. The position of the curves is important in this case because the curve is the actual toolpath. Our example file on the right gives the following endresult.
Milling along projected curves
If we want to mill curves on a curved surface, we can use the simplified option of projecting the curve onto the surface. To do this we click the following button.
We select the curves we want to project and press enter. The following window pops up.
File:Madcam project curve ui1.gif
With 'Stock To Leave' we can enter the depth of the cutting into the surface. If we keep this value at zero the toolpath will exactly follow the surface and thus won't be visible in the end product. To get a visible cut we need to enter a negative value. As long as the curves are positioned above the surface the Z-position of the curves has no influence on finished product. The following image shows the result of the example file at the right.
Milling between two curves
The 'between two curves' option is similar to the regions options. We can also define a specific area of the solids and/or surfaces to be milled. However the 'between two curves' option is a bit more flexible. If we use different milling operations within one milling job, it's possible that we need to mill inside AND outside the defining boundaries. If this is the case we should use either 'between two curves' or 'from boundary curve'. To use this option we click the following button.
After selecting two curves and pressing enter or right-click the 'between two curves' window pops up.
The default settings are in most cases sufficient. The Z-position of the curves has no influence on finished product.
Milling from boundary curve
The 'boundary curve' is also similar to the regions options. Here we can select curves that will act as boundaries. To do this we click the following button.
After selecting the curve we press enter or right-click and the following window pops up.
The default settings are in most cases ok. The Z-position of the curves has no influence on finished product. In our example file we use a curved surface and several curves as boundaries (see the image at the reight). If we look at the toolpath we notice that the toolpath goes right up to the boundary. This means that the center of the cutting tool goes until the boundary. In some cases we don't want that so we might need to adjust the position of boundary. The model doesn't have this correction so it looks like the following image.
If we do the correction of the boundaries and add a 'project curve' job we end up with the following result.
Simulation
To check if our settings will give the desired result we click the following button to see a simulation of the result.
The next window pops up.
The simulation window gives us several options to view the process and the end result. The most usefull possibility is to zoom and rotate to check al sides. Also the possibility to watch the simulation step by step can give us much needed information about the sequence of the different procedures.
After being satisfied with the simulated result we can close the simulation window and proceed to post processing the file.
Post Processing
To use the toolpath information in the milling machine we need to create a post-processor file: in our case the NCP-format. By clicking the next button we enter the postprocessing window.
The following window pops up.
Here we need give a name for our NCP-file, for easy identification of the file a studentnumber plus a 2 digit number is suggested. Furthermore we need to check a few things. First check if the 'Post Processor' is set to 'Isel_NCP_BK', then check if the 'Cutters' are set to 'Default from toolpath' and finally check if the 'Home Position' settings correspond with the startpoint we selected while preparing the file for milling (in this case 0,0,0).
If all parameters are set correctly we press the post process button and choose a file location. MadCam now starts post processing and at the right of the post window the progress is shown. After finishing the following notice appears: 'File succesfully written as....'.
Now our NCP-file is ready to be milled.
